CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

cavitating flow over a hydrofoil

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   January 25, 2011, 20:35
Default cavitating flow over a hydrofoil
  #1
New Member
 
Join Date: Jan 2010
Posts: 8
Rep Power: 7
Actone-Zero is on a distinguished road
Hi everyone,
I'm simulating a cavitation flow over a hydrofoil and I have a problem when I have large shedding of vapor structures (low cavitation numbers leading to unsteady sheet/ckoud cavitation). It seems that the simulation is doing well but in some cases it completely diverges and I have vapor everywhere in the domain. It usually start in the wake where a cloud suddenly develop to the entire domain. I double checked all my parameters (I mean pressure, boundary conditions ...) I'm pretty sure it is right.

I'm not very familiar with all the coefficients of the Rayleigh Plesset model so I use the default values, also I noticed that using a first order Euler scheme for time discretization fix the problem but I need second order...

Do you guys have any idea where the problem can come from?

Thank you !!!
Actone-Zero is offline   Reply With Quote

Old   January 26, 2011, 00:25
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,949
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Cavitation models are tricky, transient ones even more so. Any clues to the divergence? Do the residuals start to grow? The first thing to try is smaller timesteps.

The default values I think are tuned to clean fresh water, so may need some tweaks for river or sea water.
ghorrocks is offline   Reply With Quote

Old   February 3, 2011, 13:50
Default
  #3
New Member
 
Join Date: Jan 2010
Posts: 8
Rep Power: 7
Actone-Zero is on a distinguished road
Ok, thank you very much for the answer.

Concerning the time step I think it is small enough. Do the CFL need to be 1 in all cases? My average value is around 1. My time step is 1e-4s for a velocity of about 5m/s, Re=750000. I started a computation with a lower time step but it takes time.

I'm now inversigating different possible problems:
1- I've seen that the model has been calibrated for leading edge and mid chord cavitation, what happen if I increase the condensation coefficient to avoid development of vapor in the entire domain?

2- I've read in the manual the following:
It should be emphasised that if a poor initial guess is supplied with the cavitation model active (i.e., a non-zero initial vapor volume fraction), then it is possible to arrive at a physically impossible situation where most of the flow domain is cavitating.

In the initial solution, I turn off the cavitation model, however my volume fraction of vapor is not 0, it is between 1e-15 and 3e-15 , which I guess can be considered as 0 ?
However, this is exactly what happens in my simulation so maybe it is not propely initialized.

3- What about the maximum density ratio? I set it to default which is 1000, however it is much higher in my case, whatever the temperature (say between 10 000 and 40 000). Do I have to change the max density raion in consequence?
Actone-Zero is offline   Reply With Quote

Old   February 3, 2011, 18:37
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,949
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
0) Timestep - Do a sensitivity study to check the timestep size. Anything else is just guesswork.

1) No idea, never tried it. As long as you understand the model then go for it.

2) Multiphase simulations often have a lower limit on volume fraction to improve numerical accuracy. Don't adjust this unless you have problems.

3) If your density ratio is greater than 1000 then you might have to increase it. But be aware that this will cause numerical stability problems. Often cavitation models clip the density of the gas phase for numerical stability as the effect of density in the gas phase is small. This may be the case for you, in which case you can allow the density to clip on the density ratio limit.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Cavitating flow condensation problem mange FLUENT 3 August 30, 2011 01:49
reversed flow at velocity inlet / mass flow inlet ib FLUENT 1 March 26, 2007 13:11
How to change from mass flow to volume flow rate stanley FLUENT 1 February 2, 2007 07:44
Plug Flow Franck Main CFD Forum 3 September 4, 2003 05:57
Kármán vortex street in cavitating flow behind bodies in the cavitation tunnel L. Könözsy Main CFD Forum 0 April 17, 2000 13:16


All times are GMT -4. The time now is 01:23.